How do you cut the corner off a box model

[Anonymous]

I have a box model and i wish to remove just one corner . The flat plane so created would intersect on three sides and 3 adjoining edges. A chamfer if you like but across one corner point and not along a single edge.

Does anyone have any idea how this could be achieved ?

[carl_bass]

Here's one way but there are certainly others

Sketch a line on the top face

Then construct  > plane at angle at 45 degrees from that line

Then go to Modify > Split Body and there should be a second body created

Either turn off the visibility on the second body or delete it

A drop more complicated than seems necessary but it's a fairly general way to do it

[taylor.stein]

Hey LJHFUSCAD,

I think I found a quick way to accomplish what you're trying to do. Here are the steps I took:

1. With my Box modeled, I first create a construction plane that passes through 3 corners by using the Plane Through Three Points command found under the Construct Menu.

2. Select Three corners to create your first construction plane.

3. If this is the corner of the Box you're trying to remove, then you can skip to the last step! If not, we now need to offset a construction plane from the one we just created (it will be parallel). To do this, we'll use the Offset Plane command found under the Construct Menu.

4. Create an Offset Plane from the previously construction plane, and move this plane to the area you like.

5. The final step is to remove the corner of the Box using the Split Body tool found under the Modify menu. In the Split Body command, set the Box as your Body to Split, and select the appropriate construction plane as the Splitting Tool. You'll see that you now have two solid bodies in the browser, and you can delete/hide the unwanted corner.

Let me know if this helps!

Taylor

[carl_bass · Accepted solution]

And here's a slightly different way. Just make a box as a new body on top of the existing box

Then use the move commsnd to orient it to the right place

And then use modify > combine using the cut option to get rid of the corner

So there's 3 different ways and I'm sure there are more

[Anonymous]

This [box/combine] solution is great as it doesn't leave the 45deg construction line in place.

Thank you all for your input, very much appreciated.

[karyeka · Accepted solution]

Another way is to chamfer the 3 edges that come to the corner. Then select the 3 chamfered faces but not the vertex cap and delete them. This delete is delete with heal where the adjoining faces are extended to heal.

Please check the video - https://screencast.autodesk.com/main/details/fd72d356-0868-4e37-8132-755e00221f8a

Thanks,

Anand

Fusion360 Development

[Anonymous]

after few trail and errors of my own i came up with same solution. But cant we have one single option in 'modify' so that we do it in one step (as in solidowrks). am just in tremendous love with fusion 360 as i shifted from sketchup to fusion for mastering my design skills, every now and then i compete with my design engineer that who can do better things with their tool. Me in F360 or Him in solidworks. He showed me an option where he did this in one shot. Please ask your developers to add this feature.

[promm]

syedmahin1991,

In order to add the corner chamfer Fusion 360 would need the ability to apply a chamfer to a vertex.  I believe this a good suggestion and I recommend you create a post in our IdeaStation to gather support around it.  We use the IdeaStation for customer feedback as well as a way for our community to influence priorities to our development backlog.

Link to IdeaStation

https://forums.autodesk.com/t5/forums/postpage/board-id/125

Cheers,

Mike Prom